Monday, September 10, 2012

Planning is an important part of design. This is especially true if you plan on printing that design on a 3D printer, like the Cube. It's also imperative if that design must interface with a real world object.

In this tutorial we cover making just that. We plan to print at least 100 pieces of the design and that design must fit firmly onto the end of a PVC pipe.

The object that we will be demonstrating will be used in an outdoor Christmas display. It's a cap that holds a Christmas light and that cap fits onto a piece of white PVC pipe that, hopefully, will end up simulating a candle. The candles will be used to line a driveway and, ultimately, they will be joined by links of white plastic chain.

We won't get as far in the design as adding the loops for the chain in this tutorial. That is saved for the next tutorial. But, in around 11 minutes we will be able to finish the basic design of the cap. And, the reason we can do that so quickly and so precisely is that we already know our design's measurement constraints and we can guide our design using these constraint with reference objects.

Specifically, we will use several REFERENCE RECTANGLES and a single REFERENCE LINE.

Reference objects are only guides and aides for your s ketch. They do not actually control the shape of the 3D part. But, they are extremely useful, as this demonstration should attest. But, what makes them even MORE useful is our ability to easily change dimensions after the reference object has been drawn.

Here is Tutorial #16 that, hopefully, effectively demonstrates the power of reference objects when combined with MAKE DIMENSION when real precision is required.

In our next tutorial we will add the loops that are used to connect the candles using plastic chain.

For the most part, Cubify requires sketches to be closed perimeters with no intersecting lines.

In this tutorial we show how the Sketch Tools EXTEND and INTERSECT, along with ANALYSIS can work together to ensure that we create compliant designs.

FILET and CHAMFER are also demonstrated. These two commands are also available for edges on 3D objects. The work very similarly, with the difference being that FILET rounds corners and CHAMFER cuts a straight line across corners.

We also demontrate the two PATTERN Tools. LINEAR PATTERN creates an array of new objects while CIRCLE PATTERN creates the specified number of copies in an arch around a center point.

Thursday, September 6, 2012

We do a little bit differently in this tutorial. We include a brief demonstration of how Moment of Inspiration (MOI) handles the SWEEP command before looking at Cubify Invent's SWEEP. The difference is that MOI allows us to use TWO paths or RAILS along which to SWEEP our primary shape. As of right now, Cubify Invent only permits us to use a single path or rail.

But, as we shall see, while that presents some challenges, Invent's SWEEP still allows us to do amazing things.

HOW SWEEP WORKS

I like the term that Moment of Inspiration's developers use when describing the path on which the primary sketch rides. They call it a RAIL. And, that is a great analogy. SWEEP is just like a train traveling on a RAIL, following every curve and nuance of the rail as it moves from one point to another.

SWEEP starts with a sketch. That sketch can be simple or complex. But, in Cubify Invent, it must be a CLOSED drawing. We demonstrate with a circle and a curved wall as out primary objects. Think of SWEEP as an EXTRUSION that follows a path determined by an OPEN rail.

The Rail is a second SKETCH that is NOT an enclosed path. This RAIL or PATH is used to guide an extrusion of the closed, primary sketch. The SWEEP follows the basic rules or behavior of the EXTRUSION tool... except that it is rarely straight. A sketch of two Circles, therefore, can become a curved pipe and that of a single circle becomes a curved, solid rod.

We don't have time to get into all the specifics of relating the RAIL to the CLOSED SKETCH in this tutorial. We just cover the basics. But, some very, very complex curves can be created under the SWEEP umbrella. So, expect more explorations to follow.

THE VIDEO TUTORIAL

Here is the video. At just over 16 minutes, It's much longer than I usually prefer. But, the subject matter is so rich that I hope it justifies the extra time spent viewing it.

The raw power of SWEEP to create more organic features makes it well worthwhile to explore in greater depth. Plus, it's always surprising and fun to see a finished sweep for the first time. So, rest assured that there is more to come regarding this wonderful tool!

Wednesday, September 5, 2012

Come back to this post over the next few days from the origical posting date. Because, I am sure that we'll have some very cool images of applications using Helical Boss.

In this initial video tutorial we explore various combinations of shapes, reference line angles and Helix properties. Hopefully, it will whet your appetite for more.

So, let's just jump right in and take a look at the Helical Boss tool!

SAMPLES NOT ON THE VIDEO

Sample #1: Hollow Tube

This sample was based on a complex shape with a center circle. Like Extrusion, if the shape has a wall, the Helical shape will be hollow.

Sample #1 - Hollow Tube

Sample #2: Wrapped Ellipse

A cylinder was first extruded and then an Ellipse was wrapped around the cylinder.

Sample #2 - Wrapped Ellipse

Sample #3: Wrapped "Leaf"

Using the Spline Tool, a leaf shaped sketch was created and then wrapped around the cylinder with Helix Boss. The result, due to the curvature of the leaf shape is a cupped helical ornament.

Sample #3 - Wrapped "Leaf"

Sample #4: Circular Pattern Feature using a Helix

Combined with Circular Pattern and Mirror, a Helix can create very complex shapes. Here a single Helix with taper was first replicated with Circular Pattern and then Mirrored to form a top and bottom.

Sample #4 - Circular Pattern Feature using a Helix

Sample #5: Multiple Independent Shapes in a single Sketch

Sketches to be used with Helix Boss can include multiple independent objects (Not Touching). In this sample we began with 8 circles arranged in a circle. They could have been arranged in virtually any configuration as long as the independent are located where they would work alone.

Sample #5 - Multiple Independent Shapes

Sample #6: Corrugated Pipe

Buy using a polygon and a pitch that results in a slight overlap, we can create an object that looks like a corrugated pipe. A triangle, oriented the right way can also be used to create a screw.

Sample #6: Corrugated Pipe

The variety of things we can create with the Helix Boss and Helix Cut tools is, for all practical purposes, unlimited. But, care will have to be taken to make sure that the resulting shapes print well without requiring too many supports. So, this could limit the practical applications.

Even so, it's great fun to see what one can do with just a few simple changes in the combination of sketch, reference line angle and Helix properties. Have fun!

Tuesday, September 4, 2012

Before attempting to learn how to create a bolt using the Helix Cut tool, I scoured the Internet to see what it takes in other bigger name CAD packages. I also scoured the Internet for information about bolts and thread specifications. So, others unwittingly helped me as I tacked learning Cubify Invent's techniques for creating a bolt using actual specifications.

What I learned is that designing a bolt in Cubify Invent is actually EASIER than in many well-know CAD packages. That's probably because they have a legacy interface. I was surprised how easy it was to not only cut threads; but, to do so with precision.

Of course, the drawing is going to be a lot more precise than any extrusion printer can currently deliver. But, that's OK. 3D technology that is expensive today will, one day, be affordable to home users. So, all that precision will NOT go to waste.

Creating the bolt took place in steps.

STEP #1: Create the Bolt Shaft

The first step in creating a bolt is to precisely create a blank shaft at the OUTSIDE specification for the bolt size you want. In this case, the OUTSIDE of the threads would be .427". Since we wanted a bolt having 1" length for the threads, we created a cylinder that was 1.276", allowing for the head depth.

Step #1: Bolt Shaft Extrusion

STEP #2: Create the Bolt Head

The bolt that I measured as the model for the tutorial had a head that was .609" across and was .276" deep. The MAKE DIMENSION option makes getting the sizing precise very easy.

Step #2: Bolt head Extrusion

STEP #3: Chamfer the tip

Chamfering is the process of cutting an angle along an edge, By, putting an angled edge on a bolt, it makes it easier to start. In this case, we picked a random measurement of .075".

Step #3: Chamfering the Bolt Tip

STEP #4: Use REVOLVE CUT to shape the head.

This was actually the toughest process to design and implement. The process involves designing a cutting tool that trims the top and bottom of the head as it is REVOLVED around the head. The depth of this cutting tool had to be great enough to clear the pointed edges. The great thing about Invent is that you can EDIT the cutter after you try it, so that corrections can be made with automatic updates to the result. Nice!

Step #4: Forming the Head with Revolve Cut

STEP # 5: Create the Thread Cutting Tool Shape and Reference Line

Thread specifications include DEPTH and PITCH. The depth is controlled by the size and shape of the tool used to cut the threads. In this case we used a triangle that was .040" deep. This number came from one of the many specification sheets that can be found on the Internet.

At the same time, we created the reference line around which the Helix will revolve. Creating a Helix, either BOSS or CUT, always involves a shape and a reference line. The distance between the reference line and the cutting object determines the circumference of the Helix sweep.

Step #5: Create Thread Cutting Triangle & Reference line

STEP #6: Cut the Threads using HELIX CUT.

Cutting the threads turns out to be extremely easy. When Helix Cut is selected, a dialog asked for a number of parameters. In this tutorial, all we needed to enter was the length of the Helix (1") and the PITCH of the cut. The bolt modeled had a pitch of .060".

Step #6: Use Helix Cut to create the Threads

STEP #7: Finished Bolt.

Here is a picture of the finished result.

Finished Bolt

VIDEO OF THE PROCESS

I hope this tutorial video shows that using HELIX CUT is relatively easy if we remember we need and object AND a reference line. It was actually quite interesting to see how much easier this process was in Cubify Invent as compared to some other, more famous, CAD programs.

Monday, September 3, 2012

If there is one command, beyond EXTRUDE, that is probably among the most used, it would be RESOLVE BOSS. There is a good reason for the popularity of this command for both novices and experts.

For novices, it allows us to create very nice, useful designs with just a simple sketch and one command. But, the power of RESOLVE goes WAY beyond being able to create cups, wine glasses and vases.

It is especially useful for those designing for 3D printers. In one pass we can create extremely complex multi-part designs with outside and inside features that can only be produced with a 3D printer. And, in this tutorial, we explore one such design.

We also explore the CIRCULAR PATTERN command. This allows us to copy a part or parts in a circular pattern around a center point. The number of items and the degrees of spacing can be user selected. It is one of my most used operations in Moment of Inspiration and it will be equally used in my Cubify Invent designs! You'll love it!

As you may or may not be able to see, from the video splash screen, we used it to simulate an aircraft radial engine in just a few minutes time. (I see one splash screen in design mode and another on the blog page????) :)

The more I use Cubify Invent, the more comfortable I become with most of the commands. RESOLVE, both BOSS and CUT, along with CIRCULAR PATTERN are among the commands with which I have gained some confidence.

There are still some commands that I'm sorting out. They work similarly to what I'm used to doing in Moment of Inspiration. But, there are enough differences that more practice and exploration is needed. SWEEP is one of those commands. Simple SWEEPS are easy enough. But, SWEEP is far more capable than where I am now. Hopefully, we can have some useful information in the next day or two. In the meantime, there is plenty we can do with what we have discovered so far.

It's one thing to learn how to do something and quite another to actually put it into practice.

The immediate goal of these tutorials is to provide those who are evaluating Cubify Invention to be able to do some useful things within the 14 day trial period that allow them to decide if Cubify Invent is the right product for their needs. This involves showing some practical and not-so-practical examples... like our airplane.

In this tutorial, we add a canopy to the fuselage using an offset axis that we created using two points. Then we create elevators that are slightly angled using an angled plane and MIRROR.

I hope these tutorials are helpful to you. I don't pretend to be an expert. In fact, I'm learning the product in the same order as I am presenting these tutorials, while it is fresh in my experience. I'd like to hear from you whether they have been helpful or less-than-helpful. :)

Planes, Axis and Points may not be part of a printed object. But, they are the infrastructures that allow us to create those parts. Everything we created in Cubify Invent has some relationship to a plane, axis or point.

Points are unique in that we can create them outside of any existing plane. They can exist in space with no seeming connection to the other aspects of our drawing until we make a connection by using those points to create an axis or an entire new plane having no previously existing relationship with a previously existing plane.

In this tutorial, we examine some uses for points, axis created from two points and planes created from three independent points.

In the next tutorial, we use what we learn in this exercise to add new features to our airplane! Things are beginning to shape up!

Being able to precisely work from different angles when creating sketches and objects from sketches is very powerful. If we could only precisely work from front/back, left/right and top/bottom views, we'd be severely limited in what we could create.

Fortunately, Cubify Invent provides us with a lot of flexibility to work from just about any angle of our choosing by providing us with the means of creating new planes at an angle to existing planes or surfaces of our objects.

We can create a normal plane simply by selecting one existing reference plane or planar surface of an existing object. But, to create an angled plane we need to make two selections that are complementary. These combinations are:

Plane / Axis

Plane / Edge

Planar Surface / Axis

Planar Surface / Edge

Axis / Plane

Axis / Planar Surface

Edge / Plan

Edge / Planar Surface

No matter which order or combination is used, the process is the same. Select the first item and then Choose PLANE in the reference section of the toolbar. Then, holding the shift key, select the second item. The new plane will be created parallel to the selected Plane or Planar Surface and pivot on the selected Edge or Axis.

While the video tutorial neglected to include it, you are able to create multiple angled planes just as you can with normal planes.

Here is a short video that, hopefully, clearly explains the process...

It doesn't take long, once we grasp the process, to see that angled planes are something we are going to use very often.

Remember that when I first mentioned Cubify Invent, I said that I didn't want to immediately write a review because I was so familiar with Moment of Inspiration (MOI) that it would not be fair to Cubify Invent unless I had an opportunity to work with it a while. Well, I can tell you that the more I work with Cubify Invent, the more I have come to believe that it is a powerful design tool with a far easier interface than I could have imagined. I'm loving what I'm seeing and I've only scratched the surface!

Sunday, September 2, 2012

He alerted me in an email to an important new feature in the latest update to the Cubify Client software. I'm as excited to see it as he was!

Previously, the only file types that we could upload into the Cubify Client were .CREATION and .STL files. We can now IMPORT a THIRD file type into the Cubify Client!! And, that is a .CUBE file.

.CUBE File Type Added to IMPORT.

And, the importance of this is that, for the first time, we can visualize supports before we print them!

This is no small thing. Supports are sometimes a necessary thing in printing an object with our Cube. But, you already know how much I hate them and do my best to avoid needing supports if at all possible. Being able to see, beforehand, how supports might be generated, BEFORE printing, is going to be very helpful in making design AND LAYOUT decisions.

I've created an .STL file that demonstrates why I say this.

Design & Layout Comparison Drawing

The above image shows essentially the same FUNCTIONAL part in two different design configurations and two different print orientations. The only difference between the parts is that in one, the notch has a flat cut and in the other the notch is rounded. Each of these two designs has been flipped upside down so that the notch is pointing up.

STL Import View

Previously, all we had was the view of the part in its pristine form. Just as the .STL or .CREATION was designed. This tells us NOTHING about the final print when it comes to either needing supports or how those supports will be printed. That all changes with Version 1.0.24 of the Cubify Client.

.Cube File View

If we create a .Cube file and then load it into the Cubify Client, we now see the parts in two different colors. The YELLOW represents the part and the RED represents the support materials. We can instantly see that both design and orientation make a difference when it comes to needing supports.

Flat Notch vs. Rounded Notch

Let's first compare the DESIGN decision to use a FLAT notch vs. a ROUNDED notch. Notice how must more dense the support material is in the FLAT notch. The ROUNDED notch still requires some support; but, it is less dense, which should make it easier and cleaner to remove.

But, the real difference comes in using a different orientation!

Orientation Support Comparison

Notice that it does not matter how we designed the notch if we flip the part upside down to print it. Neither design needs support in the notch area. The only potential need for support is at the side holes.

Side Hole Support

That is NOT a lot of support in that hole! Had the supports been massive or filled the hole completely, then we might come to the conclusion that support is absolutely required. But, in fact, I'd be willing to print the flipped parts WITHOUT supports or raft just to see if I can get by with it.

I hope you can see how useful this new feature is going to be to save you (1) material, (2) time and (3) aggravation. :)

Saturday, September 1, 2012

OK. That is NOT a misspelled word. I couldn't resist. That play on words was just T-O-O-O good to pass up!

So, we are going to use planes to create a plane. And, I think you will be quite surprised at how simple it is!

In the video I do something a little bit different. I begin by using a different plane than my usual starting point. That is because a REVOLVE ends up creating the very same object no matter which plane I used for the sketch. So, by avoiding using the XY plane, it made it easier to see the features that we use to create the swept wing.

Also, I left in an aborted attempt at creating the tip of the wing. It was the result of FAILING to click "OK" when creating the new plane.

As I mention in the video, we have heard, over and over, the phrase, "Failure is NOT an option." But, that is anything but true when it comes to learning a new software application. Failures are not only common; but, an important and necessary part of the learning process. If one is afraid of failure, then learning is next to impossible. Thomas Edison is famous for embracing the positive aspects of failure when asked about his thousands of aborted attempts to find a material that could be used in his light bulb.

Cubify Invent is not the first product, 3D and otherwise, for which I have created tutorials on the web. And, every single tutorial was preceded by one or more failed attempts. In fact, every Cubify Invent tutorial, so far, has been the result of multiple recording attempts aborted for any number of reasons. Recovery from failure is what is important.

Perhaps I learned this from my high school participation in drama. There was always someone missing a line that caused the other actors to ad-lib to bring us back on script. And, that was reinforced in the years spent creating training, documentary and news videos where take after take is the norm.

Be patient with yourself as you try to learn Cubify Invent. It is as if inertia must be overcome where things roll slowly at first and then rapidly pick up speed. The trick is embracing the failures as the one sure path to successfully becoming a Cubify Invent expert. :)

Now for the fun. I hope you enjoy seeing what can be done with a few simple sketches on multiple planes.

Blogs of Note

Personalizing Help

As my granddaughters grew up, they would search the racks of cups, etc. at places like Cracker Barrel, gift shops and toy stores to see if they could find an item with their name on it. They always came up empty. They could never find a personalized item.

3D printing has solved that problem in our family.

But, what if you don't have a 3D printer. software or time in which to create a personalized 3D item? In that case, I would like to help. Just send me a request and, if possible, I'll try to design the personalized item for you.

Any resulting design will be made available for you and others to download from the Cubify.Com store. Designs will be priced at the lowest current cost permitted on Cubify.com.